Application of numerical modeling in assembly process.

Godal, Daniel ; Ruzarovsky Roman ; Taraba, Bohumil 等

1. INTRODUCTION

The article is focused on application of computer modeling of an assembly process in a flexible assembly cell. The article refers to a diploma work: Modeling and simulation of an assembly process of assigned work piece in a flexible cell (Debrecky 2007), which was solved at the Department of Production Devices and Systems. The numerical simulation is used for analysing assembly of a pneumatic cylinder cover. Particular assembly phase realisation and stress-strain states in the contact of gripper jaws with cylinder cover were observed. The cylinder cover is assembled by a three-jaw gripper and a rotary actuator. Three states were analysed: 1) minimal loads state, 2) maximal load state, 3) finding jaw force that produce only elastic deformation state. Assembly operation was divided to a 7 load steps. Parameters of assembly (force, moment, friction coefficient) were obtained experimentally. Building of simulation model, load-steps and stress-strain states are presented. Interpretive tool of numerical simulation was engineering and scientific program Ansys.

2. TEORETICAL BACKGROUND

Transmission of normal forces and moment from gripper jaws to the cylinder cover were modeled as a standard contact task. The contact governinig equations are published in (Zhong 1993). The friction force is given by the Coulomb friction model of normal component of gripping force (Bhavikatti & Rajashekarappa 1994)). There was elastic-plastic material model with ideal plasticity used for the cylinder cover and ideally elastic material model for the material of the gripper jaw. Total strain is given by summary of elastic and plastic relative deformations. Generation of plastic strains was evaluated by hypothesis Huber-Mises-Hencky (Trebuna et al., 2002).

3. EXPERIMENT

Loading parameters for simulation model were obtained experimentally. Experiments were proposed and realised by authors of article. Force measurement (Fig. 1b, 2. Press). Force necessary for pressing the cover into the cylinder body were measured by pressing the cover into the cylinder against a digital scale.

[FIGURE 1 OMITTED]

Turning moment measurement (Fig. 1b, 3. Turn). The cover was tightly clamped with clamp chucks. There was an arm fastened on the cylinder body. There was a 0.15 kg weight hung on the arm. Changing the distance between the weight and the cylinder was used for setting the torque necessary for the cover locking. Static friction coefficient measurement. Classical approach was used for measurement of static friction coefficient. Pneumatic cylinder was placed upside- own on a steel plate that could swivel. In a state when concurrent force system disequilibrium was impending (sliding occurred) the angle of repose was measured. Each experiment was composed of six tests. Measured values were evaluated statistically. Results are (assembly loads): pressing force 28 [+ or -] 1.15 N, friction coefficient 0.243 [+ or -] 0.008, turning moment 0.593 [+ or -] 0.006 Nm.

4. SIMULATION MODEL

Geometry of the model has been made in a CAD software Catia. Model was thereafter imported in a *.model format to the Ansys. Only one third of the cover and one gripper jaw were used for simulation. Beam elements (BEAM188, MPC184) were added to the model (ANSYS 10.0 2005). These elements enabled to apply a turning moment.

[FIGURE 2 OMITTED]

Finite element mesh was intentionally refined in the contact area. Structural elements SOLID185, SOLID187 and contact elements CONTA174, TARGE187 were used. Algoritm of contact calculating was Augmented Lagrange Method. Considered material properties in analyze were: cylinder cover, material copolymer butadien-styren, elastic modulus E = 2.2 GPa, Poison's ratio v = 0.35, yield stres [R.sub.e] = 25 MPa (Ehrenstein 2001); gripper jaw material carbon steel, elastic modulus E = 210 GPa, Poison's ratio v = 0.3.

There were three states analyzed: 1) assembly loads from experiments, 2) maximal loads (producer gripper data HGD-23A Festo), 3) prediction of loads where elastic material behaviour of cover was accepted only, Tab. 1. Every analyzed state was divided into six time referring load-steps (LS).

The first LS 1 represents sliding the gripper jaw towards the cover to the distance 1mm. In the following step was the jaw approached to the cover so the contact commenced. In the third load step was the force applied on the jaw. Following step represented pushing the cylinder cover into the cylinder body. This step was simulated by aplying a experimenaly obtained force on the lower surfaces of the cover. In the LS 5 was applied turning moment. Two folowing steps were release of loads and pulling the jaw away from the cover surface.

5. OBTAINED RESULSTS

The results of modeled states are presented in Tab. 2. Equivalent Mises stresses higher as 25 MPa were solved in the jaw material (steel).

Stress fields by assembly loads are presented. Fig. 3 shows the equivalent Mises stress field in the contact area for LS 4. In cover material was echieved Mises stress at the level yeild stress 25 MPa. The highest stress 30.326 MPa was solved for jaw body material.

[FIGURE 3 OMITTED]

The equivalent Mises stress field within the deformed zone of cover is in Fig. 4 presented. Deformed zone is ploted with scale factor 4. The sumar displacement in the section plane (Fig. 3) had maximal value 0.031 mm.

[FIGURE 4 OMITTED]

The stress-displacement dependance at point A is shown in Fig. 5. The point A is placed in the cover body and shown in Fig. 3. Effects of single load steps on the Mises stress generation at Fig. 5 is shown.

[FIGURE 5 OMITTED]

6. CONCLUSION

The assembly operation is not possible without yield stress exceeding of the cover material, shown the computer simulation. The cover shape after assembly will be in the end deformed and the contact zone will be visible. The assemble loads obtained of the experiment are for gripper HGD-23-A the working parametres. By applying of the maximal loads is the assembly proces always realizable bad the deformed contact area will be larger. The elastic behaviour of plastic cover material will be determined by applying of jaw force 13 N. The jaw force 13 N is to low for assembling of pneumatic cylinder cover with a cylinder body.

The further research will be oriented at the implantation of computer modeling and numerical simulation into assembly processes in a flexible assembly cell. The main aim of the research is the prediction of load forces solution and their surface impacts at assembled parts.

The research has been supported by VEGA MS and SAV of the Slovak Republic within the project No. 1/3193/06.

7. REFERENCES

Ansys Theoretical Manual, Release 10.0. (2005). Available from: http://www.tsne.co.kr/intra/data_center/ansys/theory.pdf Accessed 2008-06-23

Bhavikatti, S. S. & Rajashekarappa, K. G. (1994). Engineering Mechanics. John Wiley & Sons, ISBN 81-224-0617-3, New Delhi

Debrecky, E. (2007). Model and simulation of the chosen product assembly process in the flexible cell. Diploma work. MtF STU Bratislava

Ehrenstein, W., G. (2001). Polymeric Materials Structure-Properties-Aplycation, Hanser Publishers, ISBN 3-446-21461-5, Munich

Trebuna, F., Simcak, F., & Jurica, V. (2002). Elasticity and strenght II, Vienala, ISBN 80-7165-364-0, Presov

Zhong, Z. H. (1993). Finite Element Procedures for Contact-Impact Problems. Oxford University Press Inc., ISBN 0-19-856383-3, USA

Tab. 1. Applied loads

 Initiation of
Load pro jaw Jaw slide the contact Jaw force

Load step LS 1 LS 2 LS 3
Assembly load 1 mm 1.003 mm 38.4 N
Maximal load 1 mm 1.003 mm 120 N

 Pressing Turning
Load pro jaw force moment Release

Load step LS 4 LS 5 LS 6
Assembly load 9.3N 0.198 Nm 0
Maximal load 9.3N 0.300 Nm 0

Tab. 2. Maximal solved equivalent Mises stress [MPa].

 Maximal equivalent Mises stress [MPa]

Load step LS 1 LS 2 LS 3

Assembly loads 0 3.396 28.31
Maximal loads 0 3.396 31.45

 Maximal equivalent Mises stress [MPa]

Load step LS 4 LS 5 LS 6

Assembly loads 30.326 25.402 24.316
Maximal loads 39.535 37.135 24.975